 Our next session will be followed as a hands-on session by Mr. Abhushan on convection. So all of you can get ready for the session. So I hope you enjoyed the lecture on heat transfer in Nepal. The theory lecture. Now it's time to actually do what we are taught, like what we just learned in Nepal. So as you can see, on day two, we only did fluid flow simulation. Now we are going to add heat transfer on top of that fluid flow simulation. In heat transfer in open form, there is a different way to do it. There are different solvers for it. If you are only interested in heat transfer in solid, we will also be doing that. So we have a Laplacian form session at 1.15 by Krishna Khan. But this session is all about convection. So the outline of this session would be on heat transfer solvers that are available in open form. And we are going to see how convective heat transfer through a pipe can be done in open form. And we are going to use axisymmetric simulation. So yesterday, Professor Manuswita, a lecture you might have learned or saw the weight geometry. We are going to use that geometry today. And we will be also talking about boundary condition that is applied. And what kind of boundary condition are we going to use on the waste side of that axisymmetric mass. And at the end, I'm going to provide you some assignment that you can do at your own time. So there are different heat transfer solvers available in Laplacian form, when pimple form, when simple form. Since this talk is on convective heat transfer, I'm only providing those solvers that do convection heat transfer problem in the open form. So first one is buoyant pimple form. Buoyant pimple form and buoyant simple form is quite similar to each other. Only difference being that buoyant pimple form is a transient solver and buoyant simple form is a steady state solver. Now, both of these solvers are for compressible fluid and includes heat transfer, radiation, and so on. Now, CST multi-region form. CST stands for conjugate heat transfer. So if you have a heat transfer problem where heat is transferred from a fluid region to a solid region and vice versa, then you can use CST multi-region form. If you want to simulate heat exchangers, such kind of problem, then you can use CST multi-region form. Now, this is a transient solver and it also involves buoyant and turbulent fluid flow along with solid heat conduction. Now, since we are going to use buoyant simple form today, I'm going to, this is the file structure that is in the buoyant simple form. So, similar to any other cases, we have zero constant and system directory. And inside zero directory, you are seeing that there are two extra tom. Those are PRGS and then temperature. So, initially, there would be only UMP where it would be stand for velocity and pressure. Now, we have one more tom PRGS and since this problem involves heat transfer, there is a file for temperature as well. And if you see at constant, we have two extra file. Those are thermo physical properties and then G. The G file will give you, if you want to provide gravity in your simulation, you can provide, whether you want to provide gravity or not, or the direction of gravity, you can provide it in your G file. And in thermal physical properties, the properties of your fluid or your solid in your domain, you can provide in the thermal physical properties. Problems properties file is similar as before. You can provide, if you want to use turbulent or laminar, you can provide that in turbulence properties. And what kind of model do you want to use? You want to use K epsilon, K omega, that you can provide in turbulence properties. Okay. Now, this is the problem that we are going to do simulation of today is a convective heat transfer problem through a pipe. So, our pipe is over five meter long. And initially the pipe, the section of the pipe that you see in the black color, it is not heated. And we expect the pipe to be fully developed after certain length and after which we are going to heat the pipe. Now, the red section that you're seeing is the section where we heat the pipe. And before that, before this red section on the, on this black section over here, we are going to give adiabatic boundary condition. And here we are going to provide the heat flux or temperature. Now, the properties that we are going to use, the pipe will be of the radius 0.05 meter and the length is five meter. And we are the, the fluid that is flowing through the pipe is a air and we are giving the molecular weight and the density of the air and a specific heat along with viscosity and thermal conductivity. These properties will be provided in the file thermal physical properties. And the heat flux at the wall that we are going to provide is 20 watt per meter square. And the inlet fluid temperature is going to be 300 Kelvin. Now, since we are going to simulate a laminar flow, we are keeping the Reynolds number at 500. And we can, we have an empirical reason for entrance length that is 0.06 times Reynolds number times the characteristic dimension D, which will be three meter. So, after just three meter at 3.5 meter, we are going to provide this heat flux. So, this is the axisymmetric geometry in a point problem. So, instead of solving the whole pipe domain, we are only going to solve one part of it. The reason that we can do this is because our solution would be axisymmetric. That means that the in theta direction, so we have a direction. This is the r direction and we have a theta direction. And in theta direction, the solution doesn't change at all because the problem itself is axisymmetric. Because of which we are able to just simulate a part of the domain that is a wedge shape. And then just say that this solution that we get will be same in the theta direction or as the methyl direction. Again, this is the axisymmetric geometry in a conform. So, the block that we are going to create in block mesh will be of this shape. And it is necessary that the angle of that block should be at 5 or less than 5 degree for our simulation to be accurate. Excuse me, I have a question. Yes. The top part should not be curved. Why it is flat means the top part should not be curved. So, no need for it to be curved. Since this is an approximation, so if you join these small ways, you will end up with a circle. We just assume that the degree is kept less than 5 degrees so that we won't get any error in our solution. We will get error but that would be very small enough. And we just assume that this assumption. This is an approximation. Okay. Okay. So, I want all of you to go to this link b.ly358 SRMP and then download the folder HitFlox. You can just copy it. I am going to type it in the chat box as well. I am going to give you guys some time to download the file that I am going to use. So, you click on that link or you go through that link, you will end up in this one drive. And if you click on this download, you will download the HitFlox. I am going to click on it. So, it is downloaded. So, we will be using that file later on. So, right now you can just carry. We will just carry on with Alexa. So, yeah, again, if you click on the download, you will be able to download. You have to extract the GIF file. Now, if you download the GIF file and extract all the files and you can either copy it to your run directory. If you are using VirtualBox, you can just use this command and go to the downloads. However, if you are using SSL, I want you guys to use, go to this run directory and then do explorer.exe. And then copy that extracted GIF file over there. Or you can just mount your drive and go to the download. If you have confusion right now, don't worry, I'm going to show you how to do that later. So, again, this is the buoyant simple form file structure. So, let's discuss some of the important part of this file structure. This is the miss, the block miss that we have, we are using to build. So, this is how our block miss is. And we are using two blocks here. So, this is our first block and this is our second block. And for 3.5 meter length, we have one block and after 1.5 meter, we have the other block. We are using two blocks because in this block, we are providing the heat blocks or the temperature at the wall. However, in this wall or in this wall of this block, we are providing adiabatic boundary condition. This is why we are using two different block. If you want to see how this block miss is made, you can just go to the system and block miss, there you can see. Don't worry about it, we will see later on as well. Now, the boundary condition that we will be providing at the inlet, we are going to provide 0.073 meter per second for Reynolds number of 500. And this is for velocity. And at the adiabatic wall, we are going to provide no-slip boundary condition. And similarly, at the heated wall, we are going to provide no-slip boundary condition. And for outlet, we are going to give zero gradient boundary condition. This is for velocity only and for pressure, we are going to give zero gradient boundary condition everywhere. But at outlet, we are going to fix the pressure at 0 Pascal. Now, the temperature at the inlet, we are going to give 300 Kelvin. can you explain the pressure boundary condition why this is zero gradient in everywhere? Can you explain a little bit? So a pressure is zero gradient at the wall because at the wall we don't have flow in the normal direction right because this is the wall it's a no penetrating boundary condition and we don't have flow in the normal direction so if there is no flow in the normal direction that means so for the flow to happen there must be some pressure gradient right? Yes. So if there is no flow that means the pressure gradient in the normal direction is zero so at the wall dp by dx are equals to zero x by y whatever. Did you got it? Okay. Yes. Why at the inlet? Zero gradient? At the inlet so at the inlet we are providing zero gradient because we can do one thing either we can give pressure at the inlet or at the outlet doesn't matter right now we are providing zero pressure at the outlet and what open-form dodge is during the solving part it is going to this is a reference pressure since the value of the pressure doesn't matter but the pressure difference matters the flow happens because of the pressure difference delta p not because of the value of the pressure so if we are providing zero PA though during the calculation the open-form will provide some higher pressure over here let us assume five PA and for that calculation we are providing zero gradient at the inlet. But it should not be zero gradient means it is over specified means there should be the pressure difference right at the inlet that's why the flow is happening. Yeah that's why the flow is happening because of the pressure difference but we don't know that for the so there is two way of defining one is the velocity driven flow and one is the pressure driven flow so if you were to give pressure here let's say five PA then you will not be able to give inlet velocity over here that would be pressure driven flow so in such case here you will be providing zero gradient in the pressure in the velocity boundary condition why because that velocity will be calculated from the pressure difference that we are giving right now this is a velocity driven flow so we know what is the velocity yeah just let me explain this we know that our velocity is 0.073 meter per second and at our outlet we are fixing some pressure it can be zero or five this is an arbitrary value you can give it any value and it will just calculate what pressure that we have to give here so that our flow will maintain this 0.073 velocity at the inlet did you record it yes yes yes there was other someone wanted to ask you some other question hello sir yes sir in the heated wall boundary condition where you have given fixed gradient so sir how we will specify the heat flux like q by k what is k so k is the thermal conductivity q is the heat flux okay sir yeah heat flux okay sir thank you okay so if you uh let's go back yeah so q is the heat flux of the wall and our thermal conductivity is 0.0242 so what we are going to do is where we're going to give uh temperature gradient which is q if q equals to dt by dx by k we know that dt by dx must be equals to q by k so we know the value of q you know the value of k and this is how we are going to provide it in our open form so that's why i've written q by k here that is dt by dx fixed gradient this gradient is of temperature that is dt by dk okay now so the inlet temperature is 300 kelvin and at adiabatic wall we are providing jero gradient and at the heated wall we are giving a fixed gradient boundary condition which is being derived from the heat flux and the thermal conductivity which i just showed you and we have zero gradient at the outlet now this is the boundary condition this is how we provide the boundary condition of temperature in open form so at the adiabatic boundary condition is given by type jero gradient jero gradient this means that we have jero gradient as the name suggests and at the heated pipe we are giving fixed gradient and at the pipe heated length we are giving fixed gradient and the gradient that we are providing is 826.45 which is being calculated like this that is 20 divided by 0.024 where 20 is our heat flux and this is our thermal conductivity k now the back and front is of type weights so type weight is similar to the empty boundary condition that means we won't do the calculation in the direction of the weights but since this is a weights we are providing the weights weight boundary condition here so again this is the boundary condition that is being provided we have two weights that is weights pass one and weights pass two in 2d simulation you might have noticed that we are giving empty boundary condition so if it's a 2d simulation here and at this wall we would be providing empty boundary condition so this is quite similar to that this is the weights path so here we provide instead of empty weights in the direction where we don't want to do the calculation now thermal physical properties it is one of the very important file in our simulation since it contains the equation that we are going to use as well as like the parameters or the properties of the fluid that we are defining so it helps us to construct the fluid thermal model that allows us to specify the thermal physical model so let's start with this top thing so this is the thermal physical model for fixed composition that means there is only one composition in our mixer and it assumes that so it is based on density since the name rogue the x stands for enthalpy and e stands for entropy and in the mixer we are assuming that our mixer is a fixed composition and pure mixer that means there is no reaction happening our whatever variables let's say if we may we may have water or air in our mixer we are assuming that there is no reaction between them and suddenly the water will not change into air or something like that so hence we are giving pure mixer and transport property is constant transport property is constants where it means that we are assuming the viscosity is constant not only viscosity also the planet number is constant so if you want to do simulation of blood flow where the viscosity changes with the shear strain or stress then you may want to provide some other transport properties here and the thermal is this assumes that our this assumes that our specific cp and our heat of fusion is constant it doesn't changes and lastly we have sensible internal heat so internal energy is used in our solution here and there are two options available one is sensible and other is absolute internal heat so if you want to include heat of formation as well then you have to use absolute but since we don't want to use heat of formation we don't have a phase is happening right now so we are using sensible so if you but excuse me in energy section there is one option of sensible enthalpy yeah there is one more sensible enthalpy yes yeah so what is the use of sensible internal energy and what is difference means insensible enthalpy energy and sensible internal energy in this case there is two way to solve any heat transfer problem so either you can use enthalpy transport equation or you can use entropy transport equation so based on that what do you want to use you can provide it you will get approximately the almost the same answer however right now we are providing solving this equation using internal energy for most action also there is h constant e constant so when we when we use the h constant when we use e constant yeah when you use h constant you are using internal when you use e then you are you may want to use the entropy but you have an idea or scenario when we should use h constant and when we should use e constant any specific thing there are two options and it should have different huge cases yeah there are two it's just that there are two ways to do the same thing right now I cannot think of any problem whether you want to use one cases specifically but in general like most of the problem that we do you can go with any doubt you'll get almost the same answer with slight changes because of the numerical errors okay okay thank you thank you now uh if you go below to the thermal proper thermal physical properties you will get to this section where we provide our molecular weight and then equation of state we provide density and then we provide cp and hf hf stands for heat of formation that means whenever there is change of phase we need to provide heat formation right now there is no heat formation so this is just a placeholder right now and this is the viscosity and this is the pended number excuse me molecular weight is going to affect the number simulation or we can put any number so right now in this case yeah right now it doesn't affect because there is uh no heat uh like there's no phase change and we have only one uh fluid this uh we can use between simple form to simulate different mixer in such case you may want to use molecular weight in only in such case the molecular weight will affect okay thank you so the commands to uh run that file is block mess as usual which misses our block and then go in simple form which will run our solver and rise the result uh in the heat force folder and then we can finally visualize using paraform uh now i think i'm going to do is i'm going to show you guys uh the actual simulation so this is the heat flux uh file that i downloaded i'm going to extract it so it has been extracted so inside heat flux i have another heat flux block file let me open my so if you forgot any of the command that you use before what you can do is you can type history and you can go above and see what commands that you have used before this is one of the thing i use frequently so i'm going to use this command cd this thing i'm going to copy it and i'm going to paste it in a draft box this is for the people who are using double asl okay now uh what this command does is this command will uh direct you to a directory to watch your downloads here i'm using regmi because in my pc my pc name is regmi your pc name may be different it may be something else other so just you can find figure out by going to this pc and then you can go to users so here it is regmi uh in your case it may be something else we can just uh edit that part and put your pc name so if i paste enter here it will direct me to downloads now i am finally in this directory yes anybody want to ask yes sir i haven't done sir because you are installing the ubuntu os sir we are but we are we are what we are installing we are installing only the ubuntu terminal sir by you copy them by copying this path means uh i can able to copy only in the windows 11 path so can i paste or not opening sir uh actually i didn't understand if you say so i'm i'm also using double asl only this is just a thought this is not ubuntu you can see this is a window right i think okay we are on the same boat here so this is why i was providing you this command which i have pasted in the chat box so what this command does this command will direct you to your download section download directory so yeah if i am copying means it's it's copy like uh uh see uh double class class user class 9163 desktop class something's coming now sir for the error is showing that command not found c program command is not found you trying to copy something yes sir yesterday i am trying for we are using the blender directly by using the terminal sir but same command i am trying here sir it's showing command like okay sir we'll fix this issue after this uh session okay sir thank you present your screen so as i said right now we are in this directory downloads and uh so right now i'm in this file so if i want to go to my hit flux all i have to do is cd hit flux now i'm in my hit flux but since this is extracted i have another hit flux inside my hit flux just be careful of that and now i'm going to go to my actual hit flux by typing the same command and finally i'm able to see my zero constant system okay now let's be what is inside the zero i have t up and prgs i haven't talked about prgs uh prgs is just the pressure without the hydrostatic component so if you subtract p minus rho times g you'll get the prgs so it is just a different form of pressure where we have subtracted the hydrostatic term that is rho times g why are we using this it is because it is convenient so whenever you are trying to solve heat equation energy equation it is convenient to use this modified pressure instead of this pressure that we're using before on top of that say if you are using uh you are trying to solve solve some multi-phase problem so imagine there is a water and above the water there is an air so if you want to uh solve or find gradient agrose this interface between air and water so there's a certain jump in density right the density of water is in thousand and the density of air is in terms of 1.22 something so because of this certain jump the gradient will also have some so we don't want that it may cause some inconsistency in our solver so to mitigate that we are we are using prgs in multi-phase flow here we are using prgs just for the convenience so let me open the t file first okay sorry so as you can see i uh made a mistake i need to provide the proper directory here so since it is inside the t file yeah there is rho g h also did i say only rho g it is supposed to be rho g h okay so since it is inside zero i am providing the path zero as well here so now okay this is my uh t file that is inside zero it contains boundary condition for t so initially we are going to give uniform one boundary it means that when our simulation starts the whole field will be the whole temperature of my domain will be one so you might have noticed that in pressure and velocity we will provide zero but now we are giving it one why because if you give temperature at zero our solution will not solve it it's like dividing zero by zero so this won't work this is an absolute temperature so we we need to give some value any value that is greater than zero hence right now we are giving this one and this is the inlet at inlet we are giving 300 kelvin and it is uniform and at outlet we are providing zero gradient boundary condition and at adiabatic part of the wall we are giving zero gradient and similarly as i showed you in my presentation at the heated section we are giving fixed gradient and the gradient is calculated like this 82.645 this is the temperature gradient and it is being calculated by dividing q with the thermal conductivity k and at the back and front which is our wage in this case we are giving wage boundary condition now let's see the p so here we actually don't need to provide any boundary condition for p this is not even necessary without the p-file our simulation will run but we would like to see the actual pressure when we try to visualize our stimulation so the pressure p is being calculated so it will be calculated based on the the prgs value that is being actually solved in our equation so so i said right prgs equals p minus rho times g times h so prgs equals to p minus rho times g times h and now we know that prgs using rho g and h we are going to find out p this is how this calculated thing is being done so we are giving calculated boundary condition in all the passes except for back end front which is our wage pass i'm just gonna remove it and okay now we are going to see velocity so at inlet we are providing fixed value and that value is 0.073 be careful while providing this uniform see this is a vector i'm giving my velocity in the x direction this depends on your mesh how you have meshed your geometry if your inlet is in x direction you need to give it in x direction if your inlet is in y direction you need to give in y direction now at outlet we are giving zero graded boundary condition and at pipe adiabatic and pipe heated within the wall we are providing mostly boundary condition and similarly to other cases at back and front we are giving widths boundary condition okay now let's see the modified pressure so initially at inlet we would be giving zero graded boundary condition if it was just a p folder but right now we are giving fixed flux so what does this fixed flux special do it is similar to zero gradient boundary condition but it takes in account of the other body forces say gravity force right now our problem does not involve body forces like gravity but if you it if it were to involve then it takes care of that as well so that is the difference between just the zero gradient boundary condition and fixed flux pressure and at the outlet we are giving prgs pressure so before we would provide some pressure at the boundary condition pressure equals to zero but this is prgs this is not p so we need to calculate prgs based on the value of p that is being provided so at here we are providing the value of p which is uniform zero so based on the value that we have provided it is going to find out the prgs value using the same equation p minus rho times g times h so using this it is going to find out the prgs and it is going to give that value at the outlet and at adiabatic again fixed flux pressure this is similar to zero gradient as i pointed out and same at the pipe heated these two are just the walls and at back in front we have weights let me clear the screen now that we have gone through all those files at the p let's look at the constant so in constant we have g thermo physical properties and turbulence properties let's look at g first here we are providing our direction of gravity we have negated gravity for our problem that's why the value is just zero zero if you want to provide gravity let's say in z direction you can do so by by giving here 9.8 but right now we are not providing any gravity so let's look at the thermo physical properties which is the most important file so as i show in my presentation this is how our thermo physical file is so this is the thermo physical model for fixed composition that is based on density and we are giving pure mixture as a mixture that means there is no reaction that is happening in our mixture if you had like two different complete two different compositional in our mixture let's say carbon dioxide and then air there is no reaction between them but here we have only one mixture that is air so we don't need to worry about anything and in transport we are giving constant transport that means our viscosity and Prandtl number is constant like i said say if your viscosity depends on temperature or if your viscosity depends if you have a non-nuclear inflate then you can just say in this parameter there are different models that it's available in opon form you can give that over here and in thermo we are using as constant so it assumes that our specific heat is constant and heat of fusion is also constant and equation of state we are giving row constant i think i forgot to talk about the equation of state so in equation of state we can provide different parameters so row constant assumes that our density is constant here are other parameters that can apply like business approximation and the one where the temperature depends on some polynomial expression and specie is specie in specie it just means that the it specifies the composition of its constant like number of moles such kind of thing is used here so because we have used specie in here we need to only provide a molecular weight and these are just the properties of our mixture so molecular weight is 28.9 these of air and density is 1.225 we are using constant density here in our equation of state if you we have to use business approximation then we would also need to provide row and along with the row the temperature and the value of beta over here and in thermodynamics we are providing cp specific heat and then heat of formation which is zero in our case and this is the viscosity and this is the standardization number now let's look at our turbulence properties so since our simulation is laminar there's nothing to it it is just laminar we not we need not to write any other disk technique even if you wrote any other dictionary for our turbulence it will just ignore it so let's see what is inside our system so as usual we have controlled the average skin and average solution let's see how our darkness is done so this is the vertices that we are providing just remember the weight shape figure that was shown to you before that had two different blocks so this is the first block where we have adiabatic boundary condition at the wall and this is the second block where we are providing flux condition and we are not giving any curve edges that's why this is empty so this is how the inlet is defined so one may notice that how to create a weights so previously there would be a four different vertices for one phase but now we have only three so you can just repeat the value where the weights happens like at the axis of the weights we have zero and then three so you can just have to repeat it and these are the boundaries inlet outlet pipe adiabatic pipe heated we are just giving the numbering of the phase in our boundary and we are not using any Morse path phase so now that it's clear let's run our simulation so to run our simulation first first i'm going to block this which will miss my geometry okay i have not sourced my open form i have multiple version of open form in my system so if i do os 9 it will actually load open form 9 in my system you don't need to do that if you have only one version of open form so now that i've blocked it it has missed my geometry now i'm going to run purent simple form it should run my software this should take a while because we are solving now we are solving multiple equation here we have velocity pressure and then energy equation so as you can see here we have ux ui uz and e we have e because in our thermo physical properties we had given sensible internal energy and e stands for internal energy if you were to give a sensible enthalpy then it would be h here that means we will be solving energy equation based on the enthalpy so it is still being solved just wait for a while someone is asking why the value of g is zero zero zero we are not we are not considering gravity at least in our simulation right now how to pass we can just scroll your mouse if you scroll your mouse it will pass if you want to continue the space interval okay our simulation has ended and let's view our result if you are using virtual box you can just view using paraform but now we are using double echel so let's do some extra work so i'm creating a dummy file towards result.form if i do that and if i type ls now i will have this file result.form this this can be used this can be opened by para view to view our simulation result so i'm going to explorer.exe space that this will open my directory in file explorer so as you can see i am inside my download heat flux and influx so this is the dummy file that i created and i'm going to click on it open it i'm going to click on apply so this is the pressure right now we are at 100 iteration or 100 time step i'm going to view the latest time step and this is my pressure if i want to view velocity this is how my velocity is so as you can see here the boundary layer is developing and somewhere in between that is around three meters my this developing boundary layer becomes constant and we say that my our flow is fully developed let's see a temperature so as you can see the temperature is 300 because supply 300 over here the green sorry the blue is 300 and since here we have adiabatic boundary condition there is no changes temperature and finally after 3.5 meter we are providing heat flux because of which our temperature at the wall changes and we have temperature boundary layer along the wall now if you want to visualize the plot of temperature or velocity sir can i ask one yes sir when you were showing the pressure the values were very little so these were not absolute pressure they were relative pressure because atmospheric pressure is 10 to the power of five pascals this is indeed an absolute i would say absolute pressure but here it doesn't matter the value of pressure so you you want to say that the value of pressure is very less right because at the boundary condition if you have noticed at the outlet we had even zero pressure right so based on that it is calculating the inlet pressure so the value of the pressure doesn't matter if i i can provide 100 in place of zero and i would get the same result it's just that my value at the outlet will be 100 plus whatever this value over here is around 200 something okay thank you sir okay and this is the prgs this is the modified pressure that was being calculated but since our case we are ignoring gravity our prgs and p is same that's why the you see no changes and again so this is the temperature so i was going to show you guys how we can plot our value of temperature and velocity profile at any given length so first you have to click on this plot over line and instead of just typing point one and point two i want my line to be aligned so i'm just going to click y axis why i'm going to click y axis you can see the axis direction here so this is y so i'm going to click on y axis and my my line is somewhere over here i want it to be somewhere over here let's say let's type five meters since my pipe is a five meter length so as you can see the line that i'm going to plot across is over here i'm going to click on a plot so this is giving me different uh variable we have p prgs t and u magnitude some of the values are very high some are very less because of which we cannot get any information so what i'm going to do is go over here uh at my left and see these parameters and then i'm going to click on this all and i'm going to uncheck that again so that i don't have any values left so one by one i'm going to click on my the parameter that is of my interest so let's foresee the temperature so this is how my temperature is changing along my uh radial direction so initially at the zero we have 304 zero means at the center we have 300 kelvin 304 kelvin and it slowly increases to 330 kelvin let's see the u magnitude that is velocity so this is how my uh velocity is so my velocity would be a parabolic profile and since this axis symmetric case i'm only able to see half of that parabolic profile so at center i have my maximum velocity which is 0.143719 and it is parabolic in profile now let's see uh pressure so seeing pressure doesn't make much sense in this direction it would make sense if you were to uh see it in the this z direction sorry in this case it is x direction so i'm just going to click on x and click on apply so where am i at okay uh this is my point one i want it to be a zero i want to see okay i'm gonna delete it and i'm gonna plot over the line again so this is how my pressure is uh pressure profile develops across the line so initially at the entrance my pressure is very high that is 0.0249 it may not be high but it is just larger than the my zero so what we have to look is the pressure difference not the absolute value of pressure as i pointed out before so at the outlet the pressure is zero as we define in our boundary condition and based on that the pressure boundary condition at the inlet was given zero get in and based on this value of pressure it is going to calculate the pressure in the inlet and throughout my domain so that it will maintain that flow of 0.07 uh meter per second around that so this is how you simulate convective heat transfer to apply sir i have one question sir yeah you can ask me question yes sir sometimes our geometry is not well oriented in x y z direction so at that time sir we want to pull out along elly line elly line for my desired variable suppose that line is inclined so how can i draw in part of form sir can you show sir yeah i'm gonna show that to you uh it is best that you incline you make your geometry so that it is just like sir we are using influence or probe we can using probe for detect the point so yeah like that can i use here sir any option sorry i don't get your question just like in sir in case of cfd post sir influence okay sir at at that place sir we are using probe for detecting that point and drawing the line uh where we want to plot that our desired variable so how can i do here sir is there any option so like we want to draw in client line is there any option sir yeah there's an option to draw an incline line so say i'm going to delete this i'm going to do a plot over line because i don't know the diamonds uh points the location of the points but so you need to know the location of the point for that but even though you don't know there's a uh approximating that we can do we can just drag this here so if your uh orientation of your geometry is according to this it will only change in x and y direction it won't change in the direction that is perpendicular to you so as you can see when i drag this my here it is also changing so the value of z here is close to zero so it is not changing so let's say i want to uh plot across this this uh line that is not oriented to my any of the axis okay you can just make it zero and you can apply so this way also it's like it's heat and trial like that man yeah it's a heat and trial but uh but it's not a heat and trial because if you are making the geometry uh by yourself you know the value of uh what what do you want to know like you know where is my length where is my edges right all that that is the okay that is the defined thing sir suppose we want to at that wall that wall is curved so at that time i don't know each and every coordinate of that length okay so at that time it's difficult to draw here i think yeah at that time it's difficult to draw you just in case of safety post it's easy sir okay so that's why i'm okay it's okay it may it looks like heat and trial but if you know your geometry very well uh i think you will you should be able to do it and okay i'm just i'm just going to present my uh angle uh window over here so we were here last time and this is the profile that we got uh constant wall heat flux actually this is not from the para view this was extracted from the para view and then uh it was post process in excel you can use the librae office or any uh software that handles uh tables to calculate this so say if you want to extract uh this parameter say five and then hello sir yeah yeah i have a general question actually i was using open form 10 version okay and i ran your uh software okay over there so the thing was that i uh there is no buoyant simple form uh over there it has been replaced by just buoyant for simpler generals so okay now the same code which you have provided i'm not able to sort using this particular software in the open form 10 version this brings me to the general question if we have if you have any case files which we got from github or generally anything and we are uh means we want to update it as regarding the as per uh to our open form version so what changes we need to do for that uh it depends on the new version so you need to keep track of what is different and different version for that so generally from version to version there is not much difference what in uh open form 10 uh they have done some huge changes so i think what could be the issue is uh the thermo physical properties file the name of the file any of this file could be different in your open form version 10 they might have changed the name that could be the issue along with the name of the solver but generally from one version to another version there is not much different there may be a new solver that may be available in other version but most of the time they they try to adhere to the standard that was maintained before so suppose in my case uh i am getting this error when i try to run using boind form keyword pimple is undefined in dictionary home slash my run directory for the open form slash uh heat flux slash system slash fv solutions so do i need to change something in the fv solution that means there is something wrong with the fv solution instead of pimple it may have some other name in open form 10 that could be the thing uh if you have trouble this kind of trouble what you can do is just copy paste that uh error that you get in your any browser and here are we have a very good community with open form and in cfd online that we mostly use the problem that you have faced might have also been faced by some other other people and they will post the same problem in cfd online you can go there and people will be discussing in that cfd online how to solve that problem uh even if you don't find say your particular problem you can post it on cfd online you can you have to create an account for that uh you can create and post on your problem and i'm sure there will be hundreds of people trying to solve your problem so we have a very good community in open form so if you have a particular particular problem uh you'll be very easily able to uh solve it okay so thank you fine okay so as i was saying uh right now i did a plot and now if i want to extract this plot i can just uh click on this same data so what it does is uh allows me to save my the plot that i did in excel sheet or in office library so i'm just gonna make some data file click on okay so i can select the precision the number of digits after the decimal how precise i want my uh data to be so i can click on okay so after this in my heat flux i will have one more file data so either using access or excel or library you can post process your data from here also so this was done by doing the same so i calculated uh wall heat flux and this is the result of that and this is the non non-dimensional velocity profile and we have a theoretical non-dimensional velocity profile y equals to 1 minus x square and this is the one that is generated by open form uh you may notice that there is some difference or deviation at my wall this is because uh i have not used a proper expansion ratio in my wall so that the number of mesh in the wall is uh much less or much closer so if i were to use the expansion ratio and makes us that the near my wall the number of mesh is much fine than the one in my other uh i would be able to eliminate this and uh this is an assignment problem so right now we wasted much of our geometry to provide parabolic inlet profile let me go back to our geometry so in our geometry from here to here we are actually doing nothing we are just letting our floor develop to a fully developed profile so this uh so this how long this is 3.5 meter long but our heat simulation is only being done at 1.5 meter so 3.5 meter of our domain length is being just wasted to provide parabolic boundary for parabolic uh flow velocity condition so instead of uh doing simulation in this part what we can do is we can provide parabolic inlet profile directly at the inlet so this is about that this is one assignment parabolic inlet so we are going to give parabolic inlet velocity profile directly at the inlet and we will we only have to stimulate 1.5 meter of our pipeline for that and for parabolic uh inlet velocity we will not need the other uh block that was here before so we don't need this thing we can just really ignore and only the second block that was used can be utilized and this is the code to give parabolic inlet velocity let me see what is happening here previously there would be an inlet and then type would be some fixed value and then value will give uniform some value but now we have to code it and we are using coded fixed value for this thing so as a type we are going to give coded fixed value and this value we are going to give some value uniform zero this is just a place holder it won't do anything here and we are going to name our velocity profile at parabolic velocity and this is the actual code that gives the parabolic inlet velocity profile so we are going to type code and has uh this bracket and this will open c++ uh this will allow us to uh code our inlet velocity using c++ so fd path at boundary so from here we are getting the all the uh miss miss elements in our miss uh using this command paths and when we give the boundary pairs that cf we are actually uh getting the position of that miss x y and z so now the cf contains the values of x y z of each of these things so if we have different miss you know uh domain it will just give us the value each uh x y z location of the miss so if you want to uh find out the value of y or x or z what we can do is see a bracket phase i dot y so dot y bracket will give us the value of the y of that particular miss and this is the scholar uh variable that we're using our distance for the radius of our pipe and you max if the maximum velocity that we are going to provide uh to our uh parabolic inlet profile that means if this is a parabolic profile here the value of u is 0.146 at the middle now we are going to loop through the all these uh phases like all the miss in our phases this is that loop for all and we are going to give uh scholar value r in which we are going to give the value of y coordinate so c of phase i dot y will give the value of the y coordinate and finally here we are providing the value of velocity so what is this vector velocity we are giving as a vector so this is for y and this is for z now this may look familiar to you so so if i were to write it uh it would look like this u times 1 minus r by r square this is the expression for uh parabolic profile in a pipe flow this is that so this is how you give that profile so this r it is getting from here and this r is a constant that is defined over here so like this using this expression it is giving the velocity as a vector so this is the assignment problem and you can uh click on this to get that assignment i'm gonna copy paste that in the chat you can do it at your own time when you are free and this is the uh non-dimensional velocity profile that you get by using uh parabolic limit velocity and same at 1.4 meter temperature profile and finally instead of providing a fixed gradient right now in our simulation in our heated pipe section we provided fixed gradient that is temperature gradient we could also provide temperature of the wall so if you want to provide temperature of the wall this is how you do it pipe heated pipe fixed value and then you need to give the value of the temperature that you see under 10 Kelvin and like i said in equation of state you can provide different parameters the one that we used currently was row constant that means we assume the density is constant it doesn't change changes with temperature the other parameters that can be used are perfect gas so based on this equation value of pressure and temperature it is going to calculate density this will be important for density driven flow and you can also assume perfect fluid so instead of perfect gas this is for perfect fluid this is for gas and this is for fluid that is the only difference and this is a boistness approximation in boistness approximation what we do is we assume that only density is dependent on time while other parameters in our other properties of our fluid doesn't change with time sorry with temperature not time and other is icopolinomial that is density is a function of temperature it is almost same as boistness approximation here also we say that other parameters doesn't depend on temperature only density depends on temperature and that dependence is based on this some function that is a polynomial function so thank you my session has ended here if you have any question you can ask us sir in the heat flux you provided fifth gradient yeah I think there is another way providing heat flux directly without dividing by thermal conductivity the name of that boundary condition is external wall heat flux temperature yeah that's what we can do because there is information so in our thermal physical properties we have provided information of thermal conductivity so if you use that open form will automatically calculate your heat flux based on that okay so should we move on to the next session yeah I think I think we are running out of time right yeah